Working with ANSYS SOLID 272 and SOLID 273 elements

You can create ANSYS SOLID 272 and SOLID 273 elements in Pre/Post.

ANSYS element	Description
SOLID272(3)	Linear triangular axisymmetric solid element
SOLID272(4)	Linear quadrilateral axisymmetric solid element
SOLID273(6)	Parabolic triangular axisymmetric solid element
SOLID273(8)	Parabolic quadrilateral axisymmetric solid element

SOLID272 and SOLID273 elements are axisymmetric elements that support non-axisymmetric loads, such as varying pressure and temperature loads, that you apply in circumferential direction with a Fourier series. In this software, you can create these elements in both structural and axisymmetric structural analyses.

• In an axisymmetric structural analysis, you must create these elements on the XY plane. In ANSYS, this plane is referred to as the master plane.

• In a structural analysis, these elements must be planar. That means that all nodes for an element must be located in the same plane, which is the master plane. You can use the General Axisymmetric Section dialog box to specify a vector that represents the axisymmetric axis of revolution.

Defining the master plane

In ANSYS, you can define the master plane on any XY plane of a selected coordinate system, or you can use the SECDATA command to define an axis of revolution. Each element can have different master planes. For example, in a model of a crank shaft, elements that define the shaft and the rod can lie on different symmetric planes. In this software, you define the master plane by selecting a vector and a point. The vector defines the axis of revolution.

• In structural analyses, you must select a vector to define the axis of revolution.

• In axisymmetric structural analyses, the vector you select must lie on the XY plane (the axisymmetric plane). Additionally, the default axis of rotation is the Y-axis of the global coordinate system.

Note:

Two elements in two different master planes cannot share a common edge.

Applying loads to SOLID 272 and SOLID 273 elements

• In ANSYS, you can apply different pressures and temperature loads to the elements or nodes that lie in the master plane than you do to the elements or nodes in the Fourier plane. In this software, you can apply loads only to elements or nodes in master plane. When you solve the model, ANSYS propagates those loads to all corresponding element edges and nodes in the Fourier plane.

• You can only apply edge pressure or temperature loads to the edges and nodes of SOLID272 and SOLID 273 elements. This software does not check the validity of those loads. When you solve your model, ANSYS issues warnings or error messages if the loads are not correctly defined.

Considerations for defining SOLID 272 and SOLID 273 elements

• This software does not check the validity of SOLID272 and SOLID 273 elements, such as whether they are coplanar. You must ensure that all elements that reference the same physical property table:Are coplanar with the correct axis of revolution.Do not share a common edge if they lie on different master planes.

• This software displays only elements and nodes located in the master plane and does not display or generate the Fourier nodes. When you export or solve the ANSYS input file, this software writes out the NAXIS, GEN, AUTO command that instructs ANSYS to generate the Fourier nodes automatically.

Where do I find it?

Application	Pre/Post
Prerequisite	A FEM file as the work part and displayed partANSYS as the specified solverStructural as the analysis type and the 2D Solid Option set to XY Plane, Y Axis
Command Finder	2D Mesh , 2D Mapped Mesh , or Element Create with Type set to 2D

How do I

Manually creating surface effect elements

Manually creating contact elements

Create an ANSYS KEYOPT table

Learn more

ANSYS environment

Working with ANSYS surface effect elements

Applying a flame temperature to SURF152 elements

Working with ANSYS FLUID116 elements

Working with ANSYS MASS21 elements

Working with ANSYS SOLID186 and SOLID187 elements

Working with ANSYS contact elements

Working with ANSYS MESH200 elements

Modeling cohesive zones with ANSYS interface elements

Specifying user defined KEYOPTs for ANSYS

Requesting output for ANSYS analyses

Previewing ANSYS solver syntax

Customizing ANSYS input files with user defined text

Look up more details

ANSYS elements

Using ANSYS high performance computing options

ANSYS boundary conditions

Working with ANSYS SOLID 272 and SOLID 273 elements, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });